Any hints & tips on parametric design "best practice"? (in Onshape)

john_smith077

Hello

I am new to parametric design. I keep finding that when I go back and tweak my dimensions, that I am breaking the design.

Can anyone give me any tips on do's and don'ts / best practice of designing things to be re-sized.

Thanks

J

coleman

Make sure the sketch is fully defined (black). 

dennis_20

Go through ALL the tutorials and help files you can find.  Pay attention to the techniques, not just the lesson objectives.

You might be breaking you designs because you don't have your sketch lines properly constrained.  For instance you might have drawn lines that appear to be vertical or horizontal, but they are not or they are not constrained to be V/H.  Not understanding and utilizing sketch constraints is probably the single biggest thing missing from a newbie's use of parametric software.  Also, learn where to put sketch dimensions so they give you a constraint.  For instance, pick two parallel lines for a dimension instead of the line connecting them or the endpoints of the line connecting them.  If you pick the connecting line or its endpoints you'll hold that line to whatever dimension you assign, but the parallel lines might now need an additional constraint (which just introduces a lot of extra and confusing work).  However, if you pick the two sides your dimension will hold those lines parallel and separated by the distance of the assigned dimension.

You might know exactly what you intend with your sketches, but unless you take advantage of the automatic and manual constraints the software doesn't know.  Further, knowing these constraints puts you in the position to control when they are or are not applied.  For instance, if you sketch a four sided figure one time you might want it to be a rectangle, but another time you might want it to be a trapezoid.  The rectangle is easy to define if you take advantage of the automatic constraints, but for the trapezoid you'd want to avoid or break at least one of the orthogonal constraints.  Here's a good fundamental tip:  ALWAYS make your sketches fully constrained (all your sketch lines should turn black).

Little things like this will go a long way to reducing your frustration and making your designs more robust.  Since you are needing to learn fundamentals of parametric 3D modelling you might also want to expand your learning arena beyond Onshape.  I'm not advocating something other than Onshape for your modelling, just that you take advantage of the huge volume of YouTube videos for SolidWorks.  The techniques are the same.  Another resource you might look into is SolidProfessor (http://www.solidprofessor.com/training-plans/onshape/)

Glad to see your attitude toward Onshape has changed.  Welcome to the community!

NeilCooke

@john_smith077 sign up for some of Cody's webinars on the Onshape home page - he does a great one on design intent that will help you plan and understand best practices for creating robust parametric models. 

Marc_Miller

Yes, the design intent webinar had some great tips to think about if you are new to parametric modeling.  The webinars are also recorded so you can watch at your convenience, or again.
https://www.youtube.com/watch?v=XKGRUN2gACQ

viru

@john_smith077 , Kindly refer below link which will be definitely helpful to you.
https://www.onshape.com/learn/introduction-to-cad#
https://cad.onshape.com/help/index.htm#cshid=videos
http://LearnOnshape.com
https://www.onshape.com/videos/topic/essential-training
Essential training Multipart studio video tutorial

john_smith077

Yes, those videos are extremely useful. Many thanks  

I have a general question about parametric design:
If I have a model that is nearly finished, is it better to create a new Sketch or to go back and add stuff to my original sketch?

shashank_aarya

@john_smith077 Generally it depends on some conditions such as complexity of part, feature tree sequence, feature dependencies etc. In some cases I will prefer to add entities in sketches where sketch and feature dependency will not affect much and model will not crash. Even if it gets crashed it should be easy to repair by redefining the references. But whenever I feel that model could get crashed in such a way that it cannot be repaired, I prefer to add new sketch and feature.

3dcad

@john_smith077
I try to think where would I look to modify that certain thing if I come back after a year or so. + give thought to what @shashank_aarya
posted.

dbaarda

I did old-school drafting at uni using pencils and paper, and after many years in software took up OnShape for hobby 3D Printed stuff. It's interesting how the workflow and approach is completely different.

With paper, we used to use 2D drawings to design the 3D object, and you'd put as much as possible into the one drawing to help you accurately visualise and represent the 3D object. The 3D object would be the product of the drawings.

With Onshape, instead sketches are used as rough initial outlines that you then extrude into 3D shapes, and you then design the shape in 3D, filleting edges, punching holes, etc. You add little sketches as you go to refine and add features, using the surfaces of the object as the sketch planes to draw the cross-section of the cut/hole/projection/loft you need. I don't even use OnShape drawings (they are redundant when the model can go direct to a 3D printer), but I find it amusing that the drawings are now a product of the 3D object.

One of the habits I've had to un-learn is putting too much detail in sketches. Sketch areas are used for things like extrusions, and when you put too much detail into one sketch, the areas get chopped up into pieces and your extrusions have to select lots of little areas. Then later, when you change the sketch, the areas change and break your extrusion. All the interactions/constraints on complicated sketches also get tangled and hard to manage, so you are more likely to break the sketch itself with changes. It's far better to keep sketches simple, and have lots of them instead. Try to limit it to one or two extrusions per sketch.

If you need it you can put multiple sketches on the same plane, which lets you view them all together in aggregate and how they line up. You can then use constraints across the sketches to ensure they line up, and these "sketch-linking" constraints are nicely highlighted in blue and are easier to manage. This then makes it easier to isolate the sketch+area to specify your 3D projections with, and they are nicely partitioned/protected from changes in the other sketches.

Another habit to break is trying to accurately define the final cross-sections in sketches, adding all the fillets/chamfers/drafts/mirrors etc in the sketch. In my experience it's far better to just capture the basic shape in sketches, and then apply the fillets/chamfers/drafts/mirrors on the 3D model. I find it tends to make the model easier to create and change somehow, and seems to cause less breakages when you change things. It does mean the sketches in isolation often look like abstract cave art, and you have to view them in the context of the 3D object and/or other sketches for them to make any sense.

matthew_stacy

@john_smith077, to complement your efforts consider utilizing "versions" and/or "branching and merging" workspaces.  Onshape is particularly adept at this, and it really helps you recover when you do "crash" your design.  It takes the risk out of experimenting (analogous to climbing on belay versus free climbing, with the latter being much safer).

One approach is to branch off from the "main" workspace to make any design changes that may be risky.  I often call this second workspace "sandbox".  It's a place to play with ideas.  If the change is successful, merge it back into your main workspace.  Otherwise just delete the sandbox and forget it ever happened.  The nearest equivalent in file-based cad software would be to save when a change is successful, or close without saving changes when you fail.

Ste_Wilson

Initially I always tell my students, start with the full billet of material and remove. One sketch per machining operation. Like many rules once you know it you can break it!

dbaarda

I did old-school drafting at uni using pencils and paper, and after many years in software took up OnShape for hobby 3D Printed stuff. It's interesting how the workflow and approach is completely different.

With paper, we used to use 2D drawings to design the 3D object, and you'd put as much as possible into the one drawing to help you accurately visualise and represent the 3D object. The 3D object would be the product of the drawings.

With Onshape, instead sketches are used as rough initial outlines that you then extrude into 3D shapes, and you then design the shape in 3D, filleting edges, punching holes, etc. You add little sketches as you go to refine and add features, using the surfaces of the object as the sketch planes to draw the cross-section of the cut/hole/projection/loft you need. I don't even use OnShape drawings (they are redundant when the model can go direct to a 3D printer), but I find it amusing that the drawings are now a product of the 3D object.

One of the habits I've had to un-learn is putting too much detail in sketches. Sketch areas are used for things like extrusions, and when you put too much detail into one sketch, the areas get chopped up into pieces and your extrusions have to select lots of little areas. Then later, when you change the sketch, the areas change and break your extrusion. All the interactions/constraints on complicated sketches also get tangled and hard to manage, so you are more likely to break the sketch itself with changes. It's far better to keep sketches simple, and have lots of them instead. Try to limit it to one or two extrusions per sketch.

If you need it you can put multiple sketches on the same plane, which lets you view them all together in aggregate and how they line up. You can then use constraints across the sketches to ensure they line up, and these "sketch-linking" constraints are nicely highlighted in blue and are easier to manage. This then makes it easier to isolate the sketch+area to specify your 3D projections with, and they are nicely partitioned/protected from changes in the other sketches.

Another habit to break is trying to accurately define the final cross-sections in sketches, adding all the fillets/chamfers/drafts/mirrors etc in the sketch. In my experience it's far better to just capture the basic shape in sketches, and then apply the fillets/chamfers/drafts/mirrors on the 3D model. I find it tends to make the model easier to create and change somehow, and seems to cause less breakages when you change things. It does mean the sketches in isolation often look like abstract cave art, and you have to view them in the context of the 3D object and/or other sketches for them to make any sense.